Programming manual.
CNC 8070
PATH CONTROL.
8.
Circular interpolation (G02/G03).
·157·
(REF: 1709)
8.3.8 Polar coordinates. Temporary Polar origin shift to the center of arc (G31).
Function G31 shifts temporarily the polar origin to the center of the programmed arc. This
function only acts in the block that contains it; once the block has been executed, it restores
the previous polar.
Programming.
This function is added to the programmed circular interpolation G2/G3. Function G31 does
not allow for the programming of the polar radius; it may only program the angle and one
or both center coordinates.
Programming format.
The programming format is the following; the arguments appear between curly brackets and
the optional ones, between angle brackets.
G02/G03 G31 Q{end_angle} <I..K{center}>
Q{final_angle} Optional. Angle of the end point of the arc.
Units: Millimeters, inches or degrees.
I..K{center} Optional. Arc center referred to starting point.
Units: mm or inches.
G02 G31 Q25 I28 J13
G00 G90 X0 Y-40 F350
G01 X60
G03 G31 Q90 J10
G02 G31 Q180 J20
G03 X-40 I-40 J-20
G02 G31 Q270 I-20
G03 G31 Q270 J-10
G01 X0
M30
To Next Page
